Hi everyone

I was wondering if anybody already work here with turbulent combustion using Reynolds Stress model for simulating turbulence. I am experiencing problem for converging my solutions. If anybody have knowledge about that I would be greatfull. I am burning methane and hydrogen, thrue EDM and flamelet model. Regards

Hi,

The RSM models are notoriously hard to converge, and combustion models are also notoriously hard to converge. Running RSM and combustion means obtaining convergence is going to be very, very difficult.

Why do you need RSM? Almost all combustion modelling is done with k-e turbulence models (or maybe SST) so you have some hope for convergence. Don't forget SST has some curvature correction models available so can partially account for the known deficiencies in k-e.

Glenn Horrocks

Hi Glenn

Thanks for your response. I used RSM in my non-reacting case flow and it converge very well. I am using those reynold stress model because my flow and turbulence field is highly non-isotropic. I want to represent my flow bypassing boussinesq hipotesis.

Using the reynold stress model I had better result away from my inlet boundary conditions. Result are significatively better for velocities fluctuation. In case of combustion, when using flamelet model, a good description of velocity fluctuation help to better describe the mixture fraction Z and the temperature and species at the same time. I already used 2-equations models such KE with good convergence and ok results. I am hoping that RS models would enhance predictions away from my inlet B.C.

Do you have some convergence tips that would help me? regards

Hi,

Convergence tips are in the documentation (in the modelling manual, Advice for flow modelling/Monitoring and obtaining convergence). More advice is here: http://www.cfd-online.com/Wiki/Ansys...gence_criteria this FAQ is aimed at steady state flows but many of the comments apply to transient flows.

I would not be surprised if you never get RSM with combustion to converge. Don't forget the SST turbulence model has some curvature correction stuff in it so is better than k-e for some cases. I would definitely try SST with curvature correction before using RSM.

Also is DES or LES an option for you? It is likely to be far easier to converge, but the computational resources required to run it will increase.

Glenn Horrocks

Hi Jonathan,

What do you mean by not converge? Did the solver blow up or did you just get periodic oscillations in your variables? If the 2nd is the case I'd suggest running a couple of iterations backing up the variables + residuals and check yourself where this situation happens.

Please also remember, although the solver is coupled for the momentum, the RS + Energy + Combustion eqs. are solved in a segregated way. Your timestep size will also play an important role in this case. The convergence curve most likely will not be as smooth as you see in CFX-brochures.

Good luck!

cfdguy

Dear users

First, thanks a lot for your response to this thread. Really appreciated.

Here is the following. At the beginning of my master project, I began with LES of non reacting flow. After noting that I was going to much time on those transient result and it was going to be hard and long time computing, I went back to RANS equations.

Since I began I have not run RANS SST models for turbulent combustion case, because I have not notice enhancement in the non-reacting flow, when comparing with conventional or modify K-E. So I decided to go with Reynold Stress model. Maybe I should try SST of reacting flows???

Regarding, my convergence problem CFX do not stop but simply stays on periodic oscillation around 10-4 for RMS residu. I am getting a wird flame but ok for temperature. By wird i mean that the flame profile do not have any realistic profile such as in my KE 2-eq modeling. I had a look at the time step and followed the CFX convergence tip. I let the mass conservation and energy equation using longer time step. I am now running cold flow first to get the flow field of the methane inside the problem. Hopefully will help to get better convergence.

thanks a lot

Hi,

The change using SST + curvature correction you might verify using your cold flow simulation. Compare it with RSM and see what you get.

Concerning your RSM approach, I'd set all equations to use the same and low time step size. Also, have a look on your buoyancy effects and make sure radiation (participating media) is performed every time step. If you march everything together, it is likely that the solver will try to converge to a solution, based on your flow field.

One more thing, just to make sure, create a monitor point like "minVal(Temperature)@Domain" or switch on the "monitor ranges" in the exp. params. Interpret this as a sanity check. It might help diagnosing unexpected issues.

Well, those are the hints I can give you. I've been through that before.

Good luck!

Dear CFDGuy

Thanks for your suggestion. About the time steps, I followed CFX manual regarding combustion tips convergence. The where suggesting to let temperature (energy) and mass fraction having an higher time step to roughly converge. An then, with the results obtained, run one again with lower value as you suggest me. From past experiences and with value around 10e-6 I was not able to converge. I know that combustion time scale are sometimes smaller then turbulence. I will have a look a my cold flow result to have an idea and maybe lower energy time step to 10e-7.

Regarding radiation up until now I have not include radiation in my calculus, because I simulate an open burner where radiation do not participate effectively. Got that either from litterature on that burner. But do you suggest me that because it could help me to converge??? regards

Well,

If radiation is not important, just neglect it, as you're already been doing. The more buttons you push in the code, more trouble you will have converging all of them.

What is a regular time scale in your cold flow simulation? 'Cause 1e-6 and 1e-7 [s] are already very low, just as the magnitude of a true Arrhenius kinetic approach. Something else is messing your solution.

In addition, check your y+ at walls. I recall that I had some trouble in the past because I had y+ < 11 at the walls. And I was using standard k-eps. Making it coarser I could manage that problem. It seemed that the scalable wall function was not working properly with all those equations I was solving.

Good luck!